SheetMetal Extrude

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    SheetMetal Extrude.svg SheetMetal Extrude

    Menu location
    SheetMetal → Extend Face
    Default shortcut
    Introduced in version
    See also


    The SheetMetal Extrude.svg SheetMetal Extrude command extends a sheet metal plate at a selected edge face.

    It creates a simple extension along the face normal of the selected edge face:

    SheetMetal Extrude-01.png Button right.svg SheetMetal Extrude-02.png

    If an outline sketch is added it creates interlocking geometry to close a profile:

    SheetMetal Extrude-05.png Button right.svg SheetMetal Extrude-04.png

    Three profiles with outline sketches to add → three results


    Simple Extension

    1. Select one or more edge face(s) to be extended.
    2. Activate the SheetMetal Extrude.svg SheetMetal Extrude command using one of the following:
      • The SheetMetal Extrude.svg Extend Face button.
      • The SheetMetal → SheetMetal Extrude.svg Extend Face menu option.
      • The keyboard shortcut: E.
    3. Change the value of the property Datalength to adjust the length of the extension.

    Interlocking Extension

    1. Select one edge face to be extended.
    2. Activate the SheetMetal Extrude.svg SheetMetal Extrude command (see above).
    3. Add a coplanar outline sketch to the property DataSketch.
    4. Set the property DataUse Subtraction to true to create cut-outs to make room for the extensions.
    5. Set the property DataOffset to adjust the clearance around the extension.

    SheetMetal Extrude-03.png Button right.svg SheetMetal Extrude-05.png Button right.svg SheetMetal Extrude-06.png Button right.svg SheetMetal Extrude-04.png

    Three profiles → position of the sketches → results without cut-outs → final results


    • A sketch can contain more than one outline.
    After inserting a sketch, at least one of its outlines must at least touch one opposite face or the tool will fail to create any extension or cut-out.
    Just one outline touching an opposite face is enough to create extension geometry from all outlines of the sketch.
    • Each cut-out will have a cuboid shape, no matter what shape the corresponding outline sketch is.
    • Shapes other than rectangles may behave little bit strange and even though the object can be unfolded, the result will not turn out as expected.

    SheetMetal Extrude-07.png Button right.svg SheetMetal Extrude-08.png

    Three outline sketches and their resulting extensions: separate triangle plate with a rectangular cut-out, circle without clearance → unfold solid is split at an unexpected position

    • In an extension operation it is recommended to leave the property DataRefine set to true (default).
    • The extension operation with a linked sketch may fail due to coplanar issues if the face on the sketch side and the face on the opposite side are coplanar, but with opposite orientations. A small offset may help in such a case.


    See also: Property editor.

    A SheetMetal Extend object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:



    • DataLabel (String): Default value: Extend (+ a sequential number for second and following items).
      The user editable name of this object, it may be any arbitrary UTF8 string.
    • Data (hidden)Base Feature (Link): Base Feature. Link to the parent feature.
    • Data (hidden)_Body (LinkHidden): Hidden link to the parent body.


    • Database Object (LinkSub): "Base object". Link to the planar face to be extended.
    • Datagap1 (Distance): "Gap from the left side". Default: 0,00 mm.
    • Datagap2 (Distance): "Gap from the right side". Default: 0,00 mm.
    • Datalength (Length): "Length of Wall". Default: 10,00 mm.

    Parameters Ext.

    • DataOffset (Distance): "Offset for subtraction". Default: 20,00 µm.
    • DataRefine (Bool): "Use Refine". Default: true.
    • DataSketch (Link): "Wall Sketch".
    • DataUse Subtraction (Bool): "Use Subtraction". Default: false